For each assembly, we create other drawing with detail part, usully we use A3 document size with 6 parts in it.

here are pictures to show what I mean

I would like to link the balloon number (and why not the quantity) of the assembly drawing to the detail drawing so that it is easier to find part and where they go for my workers.

I don't really know how to do that. In the detail drawing, I have put a view of the assembly and add a BOM. Then in each view of the part I select properties and link the ballon to the assembly BOM. It works but the bom is not linked to the main drawing and if the pieces in each BOM are not ordered the same way, I get different number.

Also I am able to add a table in the assembly model. But how to connect it to the drawing?

I don't know if we can use macro to do that. I'm not an expert in macro but I'm not a beginner too.

You can do it (even though I would not recommend it). If you setup the drawing a certain way (there are more variations possible).

Put your assembly view and the BOM on the first page as you have shown. On the second and following page you can put your component drawing views. Now here is the trick. First RMC each component view and link it to the BOM on page one. Than you add a balloon as usual. You can use a split balloon and set it to display item number & Quantity or you can add the quantity to the balloon on the outside (fig 0).

The balloon info is a life link. Any changes to the assembly should populate on rebuild or opening the drawing. In SW 2016 5.0 there is a bug and the link to the custom property won't show but you can get around using a note with a hidden leader as shown below (fig 2).

Another way is to draw a table with sketch lines then add notes into the cells. The note leader is attached to one of the corners of the cell and then hidden (that makes sure the note moves with the cell size). Then use $PRPMODEL:"CustomProperty" to link it to the MODEL PROPERTY. Now select all sketch lines and the notes and make it a block. The notes will auto-populate, when you attach the leader of the block to your model (fig 3 - I left the first leader visible to show the principle, the black leader is the block leader). Be sure to avoid duplicate Attribute names for the notes or SW will throw you a wrench the next time you edit the block, complaining about duplicate names....

There is limitations to each version...too many to list. You will have to experiment a little.

As I said at the beginning I would not do it the way you want to simply because it's a nightmare to manage your drawing files (revisions etc.) but I can see it working in some cases. For mass production it is not suitable i would say.

Thank you for your help. I have found the ballon trick before you post your answer. Asembly drawing and part drawing are different files... But I can change this and make all my plan in only one filewith several sheet.

If I do that, I am not able to link the view of a part in sheet 2 at the BOM in sheet 1. The option is grayed... I think this solution is better in my case than with sketch.

I know it is delicate to manage this but it would help a lot my workers. We are a small company and we don't buil very big machine.

Not entirely sure what else you are trying to do. You would have to attach a sample assembly with drawing file.

You need some sort of reference in between component and assembly for a life link to work. You can certainly create individual component drawing views with notes & balloons linked to an assembly BOM as long as the component exists in the assembly linked to the BOM. Even listing the QTY per assembly is easy to do. Your chosen detailing style is difficult to adapt should things change and your company happens to grow. That's when you will run into issues as this detailing style cannot easily be automated or managed. Things like nesting, cribbing, material handling & management, quality control etc. are almost impossible to do within reasonable costs. Not to mention what happens if your detailer moves on and the next guy needs to figure out how these assemblies, drawings and components are interconnected. Adding to this you would lose functionality of pack & go, re-using existing design, revision control etc.